So last time I talked about the software I use for CNC cutting and some of the terms involved. Now we are going to take a walk through the process of getting a design from the drawing board to the cutting table…
Everything I talk about here was learned through trial and error. I am not a CNC expert so if you follow my advice or ideas you do so at your own risk!
Incidentally, I’m not actually going to talk about designing multirotors or UAV components. This article is about CNC machining itself.
It all starts in Sketchup…
I said before that I tend to design in Sketchup. I did try some other CAD tools but I had used Sketchup before and I find it relatively easy to use. I also like the fact that once I have drawn some plates I can push and pull them around to create a 3D model and visualize the finished piece.
I have learned a couple of things whilst working with Sketchup that I think are essential when designing for the CNC machine.
- In the Window > Model Info tab, set the precision to something higher than 1 decimal place. I generally use 2 places (0.00mm) for my drawings.
- By default, circles are made up of 24 segments and arcs are 12. To get a smoother line (and a smoother finished curve) when you select the required tool, type in a new number of segments. I use 96 segments for circles and 48 for arcs.
After that it is just a case of measuring lines and angles to come up with your drawing. What I usually do is draw one half or quarter of a plate and then copy and reflect the piece to achieve perfect symetry.
Once you have designed your plates or components you need to get that drawing out of Sketchup in a format that can be used elsewhere.
It’s no good just exporting a 2D image as this isn’t to scale and contains no vector information that can be read by other software. For this task I use the Flattery plugin. You can get it for Sketchup 2014 from Sketchucation.com. Flattery was originally made to allow designers to “unfold” boxes so they could be printed and reassembled. What I use it for is the SVG export function.
To do this you first select everything you want to export (I do one plate at a time for a multirotor frame). Turn it into a group or component in Sketchup. Click the icon in the Flattery menu to index the lines and then click the last icon to export to SVG. The SVG format is “Scalable Vector Graphic” and is perfect as it exports all your lines as vectors whilst retainining all scale information.
File conversion and housekeeping…
Depending on what CAM software you use this step may or may not be important. Unfortunately my CAM software cannot read a .svg format so I needed to find a way to convert the files ready for use. I was fortunate to be running a copy of Adobe Illustrator for the day job and this is perfect for working with vector graphics.
When you first open your .svg file in AI you will notice two things:
- You can’t see a lot of anything
- If you can then you will find it is always upside down!
The upside down bit is easily rectified by selecting everything and rotating it through 180 degrees to get it the right way up. What you will notice though when you select everything is that the drawing is a total mess with lines running all over the shop that you didn’t put there.
Whether this is Sketchup or Flattery I don’t know but it appears that something puts an extra layer of information into the drawing that connects vectors together. What you can do about this is using the group select tool click on one of those “extra” lines and then hit delete. This will remove that top layer, leaving your drawing intact underneath.
Another thing I do at this stage is select all again and increase the line thickness to 0.5mm as I find I just can’t see anything otherwise.
Once all this is done and I have a nice clean drawing, I save the file in the .ai format as this can be read by my CAM software.Incidentally, I also use AI to add any logos and lettering to the plates as it is easier than Sketchup and you can rotate and scale the letters better.
The toolpath is where the fun really begins. There is absolutely no way I will be able to tell you how to design toolpaths in one article but I will give you some of the things I have learnt along the way…
The first thing to do when you open your CAM software (I am using Vectric Cut2D remember?) is to tell it the size of the blank plate you will be working with. I generally use either a 250mm x 200mm or 400mm x 200mm blank. You also need to tell the software how thick your material is as well as where “home” is so it has a point to work from.I always set home to the dead center of the plate as this is easy to find and mark on the blank with a ruler before I clamp it into the machine.
The next thing to do is to actually import your AI drawings and arrange them on the blank.TIP: Always leave about 10mm clear around the edge of your blank and make sure you keep the corners free for the clamps. (Or you could simply set your material size to 10mm smaller than the real piece).
Once all your plates are in place I found that in Cut2D I needed to select everything and then hit CTRL+J to close all the vectors. This means that if I then try to select a plate outline for example it will select the whole thing rather than a single segment.
Toolpaths are created by first selecting everything you want to cut and then choosing a path style from the menu. For this type of cutting I use either drill or profile. Drill is usefull for the smaller holes whilst profile is the path to use for everything else.
Never try to cut a whole design in one toolpath. By breaking it up into different parts it is easier to monitor and check progress as well as use different size end mills for different components.
So, for cutting profiles there are a couple of different things to consider:
- Cut Depth – You want to go full thickness so I always set my depth to 0.5mm deeper than the material to allow for minor imperfections. There is nothing more annoying than finishing a long cut only to find the tool hasn’t gone right the way through. Of course this means you are cutting beyond the material so see my notes below about sacrifice boards.
- Tool – We’ll talk more about tool settings later but always select a tool suitable for the job. I use 1.0mm end mills for the finer work and 1.5mm for everything else. When you have pieces that need sharp inner corners – like the camera plate at the top left of the image – I would use a 1.0mm mill for the outline cut to get the best finish.
- Machine Vectors – Inside/Outside/On refers to how the tool will follow the line. Inside is good for slots and holes whilst outside is good for outlines. I never use on unless I need to for a specific job. As a general rule, for this type of work the direction of path would be “Climb” as it pulls the chips away from the cut leaving a cleaner finish.
- Ramp Plunge – is more for metal working so I don’t tend to use it for my work.
- Tabs – I used to use tabs but now I don’t for G10 and Carbon. I’ll tell you why in the next article. If you were going to use tabs though this is where you set the size and add them to the drawing.
I’ll add some more tips and tricks below…
Once you have created your toolpaths you need to export them to G-Code. You can add more than one toolpath to a G-Code file but I like to keep it simple and save each one separately. The output I use for my machine is “G-Code Arcs (mm) (*.tap)” and to look at is nothing more than thousands of lines of numbers and letters.
Tips and Tricks in CNC Cutting
“Dogbone” drill holes
The biggest problem with CNC machining is that the drill bits are round. They can be tiny but they are still round as they are a rotary cutting tool. Most of the time this isn’t a problem. It only shows up when you want to create high-tolerance, high-accuracy parts with tabs and slots that need to lock together perfectly. This was most obvious to me when I tried to connect a FPV camera plate vertically between two frame plates. If you cut the slots and tabs with a simple end mill the slight radius’ in the corners prevent a perfect fit.
A dogbone hole is a small hole in the absolute corner of an inner radius that allows a perfect fit by removing some material in the corner. Some CAM programs will create these automatically for you but in Cut2D I had to manually place 1mm holes in all the relevant corners. A 1mm end mill on a drill path is then used to drill the holes.
A sacrifice board is a second thickness of material placed between the workpiece and the cutting table to protect the cutting table during full thickness passes. There are only two things you need to know about sacrifice boards:
- They should be of softer material than the workpiece. You don’t want your drill cutting through and then breaking on a solid sacrifice board.
- Don’t get too attached to it as it will be replaced often!
I originally used pieces of foam board for my sacrifice boards but have recently switched to MDF as the latter is both stiffer (preventing the workpiece from bowing under clamping) and considerably cheaper than the former.
Tools and Tool Settings
It is vitally important that you get your tool settings right. I broke about 10 end mills before I realised that!
Careful tool selection and setup is something that you need to spend some time thinking and learning about. I always use 4 flute carbide end mills for my projects but I use a couple of tricks to get the results I want…
There is a time however for changing this…
The tolerances can be so tight on these machines that I found a 3mm hole was actually too tight for a 3mm screw to fit through. I could have approached this in two ways:
- I could go back to Sketchup and redraw all my holes at 3.2 or 3.4mm and start again.
- I could tell the CAM software that my 1.5mm end mill had a radius of 1.1mm thereby fooling it into shaving off that extra fraction of a mm.
Option 2 is what I am doing at the moment and it works very well!
This sets how much material the drill removes in each pass over the workpiece. As a rule of thumb you should never use a pass depth more than 50% of the diameter of the tool (the real diameter that is). Any deeper and you risk tool deflection and breakage, which is exactly what I was doing in the start!
Stepover is the overlap used for pocket cuts. It should normally be 40% of tool diameter.
Feeds and Speeds
This bit is really important. It tells the machine how fast your tool can go.
- Spindle Speed – If this can be controlled by the software then set your spindle speed here. My machine has a maximum speed of 11,000RPM and this is what I use for 99.9% of my work.
- Feed Rate – Is the speed at which the tool moves through the material. I used the FSWizard online calculator to work out my speeds. If in doubt keep these speeds low to start with. As a rule of thumb I use the following:
- 1.5mm end mill in G10/Carbon – 450mm/min
- 1.0mm end mill in G10/Carbon – 300mm/min
- Plunge Rate – Is the speed at which the drill “plunges” vertically into the material during both drill paths and the start of profile cuts. I use the same speeds as feed rate.
Always double-check your tool settings and cut depth for each toolpath as these are errors that can ruin an expensive sheet of carbon!
As a result I have a number of different entries in my tool database that are in fact for the same tool doing different jobs. Just make sure you label them clearly so you know which one to use.
If you’re not too bored by now then next time we’ll look at what happens when you put your expensive raw material onto the cutting table and press the big green button…